Have you started by going through the tutorials? They are the first place you should look for answers and knowledge on how to setup flow simulations.

Assuming you have already worked through the tutorials and understand the basics of the software, you can post a screen shot of the geometry as well as the feature tree of how your model is setup to help locate your problem.

So you have the default material as aluminum. Which parts did you add PTFE to in the version that did not alter the outlet temperature?

Have you looked at the mesh to verify that your internal serpentine features are being resolved? Without a local initial mesh or high refinement they are likely lost (although that would be the same for both materials).

And the green blocks (I presume aluminum) are conducting the heat into the system.

Did you follow the convergence of the goals? Or did you leave it as the default of 4 travels maximum before stopping? I see that you have most of your goals suppressed in the image.

Because of the size of the aluminum block you want to use a local mesh. Otherwise your entire part will have a very fine mesh and it will take very long to solve.

Create a solid body that is slightly larger than the area with your serpentine.

When you create the local initial mesh, select this body and apply the settings. Then either in the local mesh settings or through Component Control, disable these solid bodies. In this way Flow will refine the cells inside of that body, but then ignores that body so that it does not affect the flow. (if you do not disable the part it will remain a solid and prevent fluid flow).

So the PTFE inserts are purely to restrict flow and increase the contact time/distance between the fluid and the green aluminum plates, correct?

If it is acceptable as a start I would simplify to a single heat sink (1/3 of your system) and assume 1/3 of the water flow rate. This way you can make the mesh much finer without greatly increasing the time to solve. Assuming you have sufficient flow restriction that your manifold produces uniform flow through the 3 serpentines this may be a valid simplification.

The beauty of Flow is that you don't have to define the properties where solids and fluid meet, it will calculate the heat transfer coefficient and such based on the materials in contact, velocity, temperature, etc.

My guess would be that the PTFE part made the mesh a mix of solid and fluid cells (mostly partial cells) so the heat transfer was reduced to a blend of aluminum and PTFE based on their ratio.

I might start by making an alternate version of the PTFE where you eliminate the vertical serpentine paths. Keep the horizontals so you have multiple parallel flow paths, but eliminate the sinuations so that it is easier for Flow to accurately recreate the PTFE as a solid.

In this case you also could have tried skipping making an extra body for the local mesh and just using the PTFE so that any cell that touches it gets refined.

That looks reasonable for the mesh. When you look from the face I would assume you can see each of serpentine walls.

500k fluid isn't unusual. I typically try to refine my mesh so that my total is around 2M cells. For a first approximation I might dumb things down (total <1M cells) to get a rough solution in a shorter time to make sure all of your inputs and settings are correct, then refine the mesh for accuracy.

This is part of why i suggested cutting your model into 3rds and assuming uniform flow - it would drastically reduce the convergence time.

I often determine the location of maximum interest and have Flow maintain a plot of that section. In this case I would make a plane halfway between the PTFE and the aluminum. Then you could watch the temperature of the water as it flows along that face.